Set CornerOvercut to True to add an extra machining move, which will cut into inside corners that would not ordinarily be cut.
This will result in some stock overcutting but is useful in cases where machined parts
will be fitted together such as slot joints or inlays.

Custom MOP Footer

A multi-line gcode script that will be inserted into the gcode post after the current machining operation.

Custom MOP Header

A multi-line gcode script that will be inserted into the gcode post before the current machining operation.

Cut Feedrate

The feed rate to use when cutting.

Cut Ordering

Controls whether to cut to depth first or all cuts on this level first.

Cut Width

The total width of the cut. If this width is greater than the tool diameter, multiple parallel cuts are used.

Depth Increment

Depth increment of each machining pass. Determines the number of passes to reach the final target depth.

Enabled

True: The toolpaths associated with this machining operation are displayed and included in the gcode outputFalse: The operation will be ignored and no gcode or tool paths will be produced for this operation.

Controls whether to cut Inside or Outside the selected shapes.
For open shapes there is not inside or outside, so the point order controls which side of the line to cut.

Lead In Move

Defines the type of lead in move to use.

Lead Move Type: None | Spiral | TangentSpiral Angle: Used by spiral and tangents to control ramp angle.Tangent Radius : The radius of the tangent lead inLead Move Feedrate : The feedrate to use for the lead move. If 0, Cut Feedrate is used.

Maximum distance as a fraction (0-1) of the tool diameter to cut in horizontal transitions.

If the distance to the next toolpath exceeds MaxCrossoverDistance, a retract, rapid and plunge to the next position, via the clearance plane, is inserted.

Milling Direction

Controls the direction the cutter moves around the toolpath.

Conventional | Climb | Mixed

Name

Each machine operation can be given a meaningful name or description.
This is output in the gcode as a comment and is useful for keeping track of the function of each machining operation.

Optimisation Mode

An option that controls how the toolpaths are ordered in gcode output.

New (0.9.8) - A new, improved optimiser currently in testing.Legacy (0.9.7) - Toolpaths are ordered using same logic as version 0.9.7.None - Toolpaths are not optimised and are written in the order they were generated.

Plunge Feedrate

The feed rate to use when plunging.

Primitive IDs

List of drawing objects from which this machine operation is defined.

Roughing / Finishing

This property is currently used only by the Lathe and 3D Profile machining operations.

Roughing Clearance

This is the amount of stock to leave after the final cut.

Remaining stock is typically removed later in a finishing pass.

Negative values can be used to oversize cuts.

Side Profile

A composite property that enables the creation of pseudo 3D
objects from 2D shapes by creating radii and slopes.

The pulley number or dial setting of the spindle for the target speed.

Spindle Speed

The speed in RPM of the spindle.

Start Point

Used to select a point, near to where the first toolpath should begin machining.
If a start point is defined, a small circle will be displayed at this point when the machining operation
is selected. The start point circle can be moved by clicking and dragging.

StepOver

The cut is increased by this amount each step, expressed as a fraction (0-1) of the cutter diameter.

Stepover Feedrate

The feed rate to use for crossover moves.

Stock Surface

This is the Z offset of the stock surface at which to start machining.

Style[New! 0.9.8]

Select a CAM Style for this machining operation.
All default parameters will be inherited from this style.

Tag[New! 0.9.8]

A general purpose, multiline text field that can be used to store notes or parameters from plugins.

Target Depth

The Z coordinate of the final machining depth.

Tool Diameter

This is the diameter of the current tool in drawing units.

If the tool diameter is 0, the diameter from the tool information stored in the tool library
for the given tool number will be used.

Tool Number

The ToolNumber is used to identify the current tool.

If ToolNumber changes between successive machine ops a toolchange instruction is created in gcode.
ToolNumber=0 is a special case which will not issue a toolchange.

The tool number is also used to look up tool information in the current tool library. The tool library is specified
in the containing Part, or if this is not present in the Machining folder level. If no tool library is defined the
Default-(units) tool library is assumed.

Tool Profile

The shape of the cutter

If the tool profile is Unspecified, the profile from the tool information stored in the tool library
for the given tool number will be used.

EndMill | BullNose | BallNose | Vcutter | Drill | Lathe

Transform

Used to transform the toolpath.

Warning! This property is experimental and may give unpredictable results.

Velocity Mode

Instructs the gcode interpreter whether or to use look ahead smoothing.

Constant Velocity - (G64) Smoother but less accurate.Exact Stop - (G61) All control points are hit but movement may be slower and jerky.Default - Uses the global VelocityMode value under machining options.

Work Plane

Used to define the gcode workplane. Arc moves are defined within this plane.
Options are XY | XZ | YZ